Working with Hole Features

Overview

Hole features are a simplified version of Form Features. In the image below you can see different features, which have only thickness faces (the SMCONVERT command respects these rules):
  • Orthogonal holes are hole features.
  • Simple non-orthogonal holes are hole features.
  • Chamfered orthogonal holes are form features.
  • If the hole thickness face consists of 2 different regions, it is a form feature.

Hole features are recognized by the SMCONVERT command if the SMCONVERTRECOGNIZEHOLES user preference is ON.

The following basic operations are allowed for hole features:
  • SMDELETE, SMDISSOLVE, disable and SMSELECT them using commands or in the Mechanical Browser for Sheet Metal.
  • Form Feature Modes in the SMUNFOLD command, including Symbol mode.
  • Associate your own 2D geometry in a flattened layout.
  • Hole features are preserved by the SMREPAIR command. Plain hole faces become orthogonal. A hole feature of the same geometry is not affected by the SMREPAIR command.

Recognition of Arrays of Hole Features

When hole features exist in a body, the SMPARAMETRIZE command detects rectangular arrays of holes on flanges, according to the following rules:
  • Holes belong to the same flange.
  • Holes are on a rectangular grid.
  • There are no gaps (missing elements) in the array.
  • Holes are equally oriented.
  • The minimal array size is either 1x3 or 2x2.

Let us illustrate the workflow on a part with Flange and Bend features.

  1. In the Settings dialog box, go to Sheet Metal/Commands.
  2. Enable the Recognize holes option for the SMCONVERT command.
  3. Enable the Convert holes to array and Parametrize holes options for the SMPARAMETRIZE command.
  4. Run the SMCONVERT command.
  5. Do one of the following:
    • Click the Convert to Sheet Metal tool button () on the Sheet Metal toolbar.
    • Click the Convert to Sheet Metal tool button () on the Sheet Metal ribbon bar.
    • Choose Convert to Sheet Metal in the Sheet Metal menu.
      You are prompted: Select 3D solids or [Entire model] <Entire model>:
  6. Select the 3D solid to convert.
    You are prompted: Select 3D solids or [Entire model] <Entire model>:
  7. Press Enter to convert the 3D solid to sheet metal part.
    11 hole features are recognized on the part.
  8. Run the SMPARAMETRIZE command.
  9. Do one of the following:
    • Click the Parametrize tool button () on the Sheet Metal toolbar.
    • Click the Parametrize tool button () on the Sheet Metal ribbon bar.
    • Choose Parametrize in the Sheet Metal menu.
      You are prompted: Select 3D solids to parametrize or [Entire model] <Entire model>:
  10. Press Enter to process the sheet metal part.
    The command reports must look like the one below:
    Created 4 distance constraints
    Created 3 fix constraints
    Created 0 coincident constraints
    Created 0 tangent constraints
    Created 0 rigid set constraints
    Created rectangular array 2x2 basing on Hole_3 feature
    Created rectangular array 2x2 basing on Hole_7 feature
    Created rectangular array 3x1 basing on Hole_9 feature
    Total: 7 constraints and 3 array(s) created
    Note: Feature names and constraint distribution may differ depending on the BricsCAD version.
    To examine the arrays, you can temporarily unfreeze the BC_SUBTRACT layer.
    In the image below the arrays are colored manually.
    Note: The green and yellow arrays are not unified. Otherwise the array would have missing holes.
  11. Edit the Array Properties in the Mechanical Browser.
    In the image below the following has been modified:
    • Green array: number of rows and columns from 2x2 to 3x4.
    • Yellow array: X and Y spacing.
    • Red array: number of rows and columns from 3x1 to 5x1.